How to apply thermal an mechanical load at the same time? 3

[JonathanSi]

Hi guys,

I have some test results and now I need to model the test in ABAQUS to compare the model with the test results. The duration of the test was 30 minutes.
I have a simple single span girder with a mechanical and a thermal load at the same time.

The mechanical load is static and applies in the third points of the beam. From minute 1-15 the load is 2x60kN and from minute 16-30 the load is reduced to 2x15kN.

The thermal load is time-dependant and applies on the whole beam from all sides. The temperature curve is supposed to follow the standard curve form Eurocode (it looks like this: T= 20 + 345∙log10∙(8∙t+1))

So far I created two steps for the mechanical loads, but now I dont know how to apply the thermal load. Can anyone help me with that?
You can find my model on following link:

https://www.dropbox.com/sh/bjqje86nlsf3bv6/AABYqddETblvsGjU60nY8krEa

Cheers, and thank you very much for your help.
Jonathan

 

[corus]

Run a separate thermal analysis and then load the temperatures in the static model using a predefined field in the load module. You probably need an amplitude curve to define the fixed temperatures with the known temperature dependent field. Run the static model using the same total time as the thermal transient as it makes it easier to understand.

I'd also improve your mesh so you have a better aspect ratio rather than the long slender elements you have now.

 

[DanStro]

I normally would do as corus suggests but if you really want to keep just one results file you can make your steps coupled temp-displacement. It may take longer to finish because of the extra (unneeded) overhead but you will end up with one odb file.

Han primo incensus

 

[JonathanSi]

Thanks for your fast reply guys. It is a great help.

@DanStro: I was trying to do what you recommended, but unfortunately I need to know the magnitude for the heat flux...that really confused me. I chose body heat flux, but how am I supposed to know the value....? The heat flux depends on temperature-differances, which I dont know and is time-pependant.

 

[JonathanSi]

@Corus:
If I first run a thermal analysis, and then the mechanical while adding the results of the thermal analysis how does ABAQUS qualculate the end result. I mean what I need is a not linear analysis with interaction between mechanical and thermal.
By simply putting two analysis together I am excactly not doing what I want to do. The research is all about the interaction between mechanical and thermal, ow they influence each other.... Do you understand what I mean?
Hopefully I missunderstood what you wrote and I am wrong

Cheers

 

[corus]

If the temperature distribution depends on the deformation of the structure, say when you have radiation between two surfaces at a certain distance apart or when contact on deformation produces conduction, then use a coupled temperature displacement model. Another case would be when you have axisymmetric geometry or when generally modelling cylindrical walls, then the temperatures are affected by the radial displacements, albeit negligibly. Or if you just want everything in a single odb then do as DanStro suggests.
When the temperatures are uninfluenced by the deformation then it's the usual practice to run the thermal separately and include it as a predefined field. The temperatures will change the deformation both by thermal expansion and by changes in material properties, if you've defined these as being temperature dependent. Stresses will be created by any restraint on the structure that prevents thermal expansion, together with your mechanical loads.